How to make a family of similar parts?

[rbtyod]

Let us say that I want to make a collection of extrusion nozzle plates that must all fit the same extruder.

The details of how the plates mate up with the extruder will  remain constant but, the shape of the opening will be different for each plate.

I would like to define a "blank" plate to fit the extruder and then create and modify openings in the copies independently to extrude the various shapes.

In a similar manner, I would like to be able to create a complete, new set of plates with the same nozzle shapes to be used on a different extruder (with different plate interface requirements) without having to redraw all the same openings.

After reading about F360's concepts of Bodies and Components I remain puzzled as to how I could best use F360 facilities to meet these requirements. I feel like I must be missing something obvious but I don't know what. I know I can make the "blank" plate as a component that fits the extruder and copy it but, as soon as I start to cut an opening in one copy of that component, the same cut appears in all the copies. I also know that by copying the blank as a body, the openings can be cut independently but, this makes it impossible to modify the complete family of plates at once to fit a new extruder.

Let us also assume that "inserts" are not a valid alternative.

Please help me understand what I am missing.

...Bob

[Oceanconcepts]

What you need to do is to to use the “Paste New” command. That will create a new component which you can edit without altering the source. 

If you are in Direct Modeling, you also have the “Make Independent” option available to break the link between components. 

Either option should give you the ability to do what you want.

[rbtyod]

Oceanconcepts, thank you for your reply.

I was aware of "Paste New" but not of "Make Independent".

Neither of these commands, however, seem to be exactly what I am looking for.

I was hoping to find a means of allowing "one way" inheritance of modifications between components.

Going back to my hypothetical extruder nozzle example, I was hoping that F360 might allow me to create a family of parts that would automatically inherit changes from the "parent" extruder interface part of the design while allowing the "child" nozzle openings to each have their own, unique designs and that any changes to the parent interface design would automatically propagate to its children while changes to the openings in the child designs would remain unique.

The basic problem, as I see it, is that F360 does not allow "one way" inheritance between designs - only exact copying with uncontrolled, two way propagation of changes.

To make a software analogy, object oriented programming with inheritance would be impossible so that every object type would have to be uniquely and repeatedly defined from scratch rather than as a modification to an already existing object type.

...Bob

[HughesTooling]

If you make your base component using User Paramaters for all the sizes you can use Paste New but you still have control over the basic size of the nozzle. 

I've attached a simple example file.

Mark

[Oceanconcepts]

I understand.  That’s a bit more involved, but what Mark suggests should allow you to do what you want with user defined parameters. There is also a future capability on the timeline for branching designs that should be able to accomplish this.

[TrippyLighting]

That functionality is called "Configurations" in many other CAD software packages e.g. Solid Works or Geomagic design.

in Fusion 360 , as has already been mentioned this will be covered When design Branching and merging will be introduced.

[JamieGilchrist]

HI Bob,

there is a way you can get most of the way there.  I would not promote this as a primary workflow, but you should be able to get the results you are looking for.

I'll take you through a simple example of what I did.

I created the common set of features that I wanted to propogate to multiple designs at the root component.

I created a new component for my first design option

Next activate the new component and copy and paste the body at the root level into your new component.

in the context of the new component, Component1, you can add features to your existing base design.

two things to be sure of:

1.  that your sub component is active to make changes and design variations.  If the root, or head of the browser is active, any modeling will likely be done on your base design.

2.  if you need to make changes to the base design that you want to propogate through the model you have to roll back your timeline to before any copy/paste actions in the subcomponents.

This method requires you to be fairly diligent about component creation and activation and controlling when and where features are created.

a word of caution about this method, too:  if your intention is a small number of variations then this may work, but as you add complexity and number of variations increases there could be an impact on performance.  I wouldn't try to guess what that threshold is, but you'll decide where this starts to break down and what your tolerance is to deal with the performance tax.

with this method in mind you could als try building your base design as a seperate Fusion item and insert it into as many new designs as you like to get all the variations you're looking to create.  With the base design externally refernced performance on each discrete variation should be a non-issue.

hope this helps and I'm happy to answer more about this technique.

[rbtyod]

First, thanks to all who have taken the time to reply. I appreciate your efforts.

I feel that I still have not made myself clear about what I hope to do. At the risk of beating a dead horse yet again, let me add some requirements to my original extruder nozzle example that may help to clarify the problems I hope to solve.

Assume that both the mount and the nozzle are not simple push-pulls of a few sketches. There are multiple, complex operations required to build both the mount and the nozzle. Having to repeat these operations manually for each specific part of a large family of parts would be very error prone so inheritantce by simply repeating sketches is not practical. It is also necessary to create multiple families of parts - one brand of extruder may use a simple round mount, another brand  of extruder may have a recessed, grooved square mount. Finally, the extruder opening is not necessarily a simple push-pull operation. Depending on the cross section of the opening, some may require special cooling passages in a specific area and so, again, having to rebuild the same nozzle model for each brand of extruder - even from a common set of sketches - would be error prone and time consuming.

While I realize that the background of most people reading this forum is mechanical design and not software, the best analogy I can think of is the Python language's concepts of base classes and multiple inheritantce that allow software objects containing features of multiple base classes to be easily and reliably combined. 

...Bob

[rbtyod]

@JamieGilchrist

I am sorry that I could not understand your post. The pictures were too small for me to read the text.

If, after reading my most recent post you feel that your suggestions are still applicable, you could attach your .f3d file?

...Bob

[TrippyLighting · Accepted solution]

Nope, you've made yourself perfectly clear.

If those  workarounds descibed above don't work for your more complex geometry, the functionality you are looking for is not yet integrated into Fusuion 360.

However, as you are mentioning software - I write some C++ for embedded controls - I am sure you are familiar with GitHub. As I already mentioned above, usualy what you are looking for in one traditional CAD packages such as Geomagic design or Solid Works - I've a combind experience in these packages of 15 years+ - that feature is called "Configurations". You have some base feature however complicated it may be that you can create derivatives off. In Solid Works IIRC you can even create sub-derivatives.

Fusion 360 as a cloud based platform, however, will ba taking that a step further and roll out a Github like version control where you can create and fork different designs off of a base design and also merge back together different design branches. This will provide you with the functionality you are looking for.  

Of course that does not help you right now, but perhaps you can share your design so we can dsicuss specifics and whether the workarounds posted above would work for you until the featurese I described in fact are rolled out.

[rbtyod]

@TrippyLighting

Thanks for the reply.

I will look forward to that new, improved F360.

...and try some workarounds in the meantime.

...Bob

[Oceanconcepts]

I think what would be needed is to clearly define what the common elements are- what is the base that is common to all, then if you branch off into differing mount designs, for instance, you can create those changes to make separate families of parts with specific mounts. The same would apply for other design elements, such as cooling channels. Essentially creating distinct building blocks. It should only be necessary to build each element once. It might take some careful thinking through order of operations if elements are defined parametrically- i.e. a cooling channel that is midway between two faces, where the dimensions of the faces might change. 

It’s hard to make recommendations without having a better picture or example of what you are trying to achieve, but my feeling is that so long as you can separate design elements that are common to groups of parts you want to create, you should be able to come up with a way to create each of those elements only once- one set of sketches, one set of operations. That the parts are complex shouldn’t be an issue except potentially with performance if you have a lot of distinct components in the same design file. 

This will be much easier when branching and merging is integrated into Fusion, but with some creative thinking about creating “objects” a workaround should be possible. 

I think you will find a lot of software people on the forum- CAD is a sideline for us, our main activity is embedded systems design. 

[jodok.schaeffler]

Has there been any progress towards a 'Configuration' functionality within Fusion 360 since 2015?

I am trying to solve the following problem:

A house design is using windows of the same type (identical frame formats), however with varying sizes, such as width and heights. The 'master' window is a parametrized design, with 'Height', 'Width_Window', and 'Width_Door' as parameters defining the height, width of the window, and width of the glass door, respectively.

The idea is now to set these parameters for every instance of a window, derived from the 'master' window, specific to this one instance. Doing this by using the 'Edit In Place' function seemed a logical step. 

Now, as you already can guess, what actually happens is that the parameters are acting globally, and with that all the instantiated windows have the same height, width of the window, and width of the door, which is the last entered value for the respective parameter.

I tried to work with other concepts in Fusion 360, such as Insert Derive (creates instances in the top level only), however, could not find a solution to this problem.

How would you be able to do a complex design in Fusion 360, e.g. a house with twenty+ windows (... I agree, this is not really complex) without this functionality? Is there anything I am missing? 

There was discussion of using GitHub for branching - is this available?

What else could help me to solve this problem?

I attached a simple model of the described setup to this message.

Tahnks for your help!

Jodok Schaeffler